- Hey there. Welcome to the first episode
of our new series Haas U where we tap into the
talents and experience of the folks here at Haas to bring you easy to understand
topics that will help you get your machining done better. I've come here to our tool crib to grab a handful of twist drills so we can talk about their differences and how to select the right one. Hey Richard. - Here you go. - Cool thanks a lot. - You're welcome. - Take it easy. Let's head out to the photo area and check out how these drills work. (electronic music) When it comes to twist drills, selecting the right one
can be overwhelming. From cheap no-name drills to high-end special helix, solid
carbide through-tool drills, the choices can seem endless. In this video we're focusing on getting value from your
drilling operations. With the basic knowledge you need to select the right drill and some tips for getting the most out
of each of your drills. So let's get started. Three basic things separate
one drill from another. Material, coating, and geometry. Let's start with the material
your drill is made from. High-speed steel is the most basic, least expensive general
purpose drill material. It's very forgiving in drill press and hand drilling operations. And they can be resharpened
to extend their life. Next is high-speed
steel with cobalt added, which holds up better than
generic high-speed steel. Cobalt gives high-speed steel
more heat and wear resistance. And these drills can still be easily resharpened similar to high-speed steel. Carbide is the most expensive but longest lasting drill material. There are different grades
with the most expensive drills usually giving the
heat and chip resistance. Carbide also allows for
coolant through-holes to be added to the drill. These through-tool drills are primarily for deeper holes and
tough to drill materials with a high pressure
coolant flowing to the tool flushes chips out much better, keeps the cutting zone cooler, and provides extra
lubrication to prevent wear. While all of these drills will
cut a hole in most materials, the carbide drills will outlive cobalt by a factor of ten or 20 times
in a rigid CnC machine. In other words, if a cobalt drill will cut 100 holes, the carbide drill will cut 1000 or 2000 holes before it needs to be resharpened. Here in the factory, with a
properly dialed in drilling op, we have examples where we're getting 5000 plus holes in cast
iron from just one drill. All that said, a carbide drill can easily cost ten times
more than a cobalt drill. So the investment is a lot higher. Despite the high price, the cost per hole when using carbide will
usually be the lowest since it can produce so many more holes. Also because carbide
is typically capable of running three to five times faster, the decreased cycle time
to produce those holes goes right to your bottom line. Now let's talk about selecting a proper coating for the
material you're drilling. This decision can really
influence performance. I've lined up a few
examples here on the table so we can get a good
look at the differences. Bright finish is the cheapest option and fares well in certain applications. For example, low carbon steel and aluminum can both be drilled with a bright finish tool usually without problems. Black oxide provides an
advantage over bright finish in that it has a bit more lubricity, offers resistance to oxidation, and additional heat treatment that can offer upwards of 50% longer life while still keeping
your tooling costs low. Titanium nitride, abbreviated TiN, is the most common coating. It is a great entry level coating for applications where lots of heat won't be transferred to the tool from cutting harder or tougher materials. You can tell titanium nitride
by its bright gold color. Titanium carbo-nitride
coating, abbreviated TiCN, is a step up from TiN. It provides a higher surface temperature, Slightly harder and
better wearing than TiN. It's typically blueish or purple in color. Finally, titanium aluminum
nitride, abbreviated TiAlN, has a much higher surface temperature rating than TiN or TiCN. This gray colored coating
is excellent for your high temperature materials, and still a good choice for steels
and stainless steels. But because of the aluminum content it isn't a good choice
for drilling aluminum. Beyond these common coatings, many manufacturers have proprietary ones of their own that tout features like high lubricity and extremely high surface temperature range. Here at Haas we use TiN coated drills mostly when we're working mild steel, for the increased hardness and heat resistance equals long life. We move up to TiCN coatings for drills used on cast iron where it shows good toughness and resistance to chipping. And when we're cutting high
strength harder steels, we'll step up to the
high end TiAlN coatings to handle the heat and high stresses where the coating helps reflect the heat back into the chips, away from
the tool and the work piece. Generally, unless you're
cutting difficult materials, a good quality cobalt drill
with a TiN or TiCN coating is a relatively inexpensive
way to get higher productivity. Also do some shopping around. Pricing varies a lot and you can find drills with high end
coatings at decent prices. So we've talked about
materials and coatings. The third key ingredient to choosing the right drill is geometry, which plays an equally important role
in drill performance. Probably the most obvious aspect of drill geometry is the drill's length. Drills come in two common lengths. Screw machine length, commonly referred to as stub length, and jobber length. When it comes to drilling on a CnC, stub length drills are
the most common choice because they are more rigid. There are, of course, all kinds of custom lengths available
for special applications. As with any cutting tool, you wanna use the shortest drill length possible because the shorter the
bit, the more rigid it is. Just make sure you have
enough flute length to get the chips out of the hole. Turns out this is geometry
question number two. How much flute length do you need for the hole you're drilling? Ideally, you want two
times the drill diameter in flute length above the hole when the drill is at the
deepest point in the hole. This allows for chip evacuation. Less than this and chips can pack up inside the flutes and
cause poor surface finish, hole size, and straightness issues. Or worse, they break the drill. But you also don't want a
long jobber length drill with flutes all the way up if you're just drilling shallow holes. This drill won't be as rigid and will yield less precise hole position. The drill point angle is probably another familiar aspect of drill
geometry for most people. When you're drilling
metal on a CnC machine you're generally choosing between 118 degree point and a wider
135 to 140 degree point. The 118 degree point is most common on general purpose,
high-speed steel drills made for cutting mild steel, aluminum, and other soft metals. And it's what you'll usually find on regular, jobber length drills. The 135 degree point is more typical for stub length drills and CnC machining and harder, tougher materials. Here at Haas, almost all the drills we use have 135 degree points when we're cutting cast iron and harder steels. Next up, we wanna consider
the helix angle of the drill. This important for proper chip clearance. Typically helix in the 30 degree range are used for general purpose
drilling in most materials. Most of the time these
will work just fine, and you won't need to concern
yourself with other options. But if you're application calls for some specialization, small
helix angles below 30 down to around ten degrees, are usually selected for harder
steels and aluminum alloys where good chip evacuation,
fracture resistance, and edge strength are important. On the other end, large
angles up to 40 plus degrees, are often used for drilling
difficult to machine materials like stainless steel where
low torque requirements and cutting resistance help cut these tough gummy metals. Last on our geometry list
is a self-centering point. This is found on many cobalt drills and almost all carbide drills. This eliminates the need
for a starting drill and helps drill in true position. Regular, high-speed steel drills aren't usually self-centering. Since it's more time consuming and expensive to grind
them with this feature. Because of this they
tend to walk or wobble when they are trying to
cut into a flat surface. More expensive cobalt and carbide drills are ground with this self-centering point allowing them to start cutting very easily with very tool pressure. This virtual self-centering
means there's no need for a spot drilled hole. And it's another way
these expensive drills can be more productive than
their economical brothers. Not spot drilling every hole
saves lots of cycle time. Okay we've looked at the basics: materials, coatings, and geometry. Now let's get into some
specific cutting condition and application related tips. As we mentioned, drill manufacturers could put holes through
the drill so coolant can get delivered right
to the cutting edge down in the hole. This keeps the cutting zone cool, lubricated, and greatly
aids in chip evacuation. Typically, steel drills
without through tool coolant can only drill about two or
three their diameter deep before requiring me to
peck-drill to remove the chips and get more coolant
down in the cutting zone. Good carbide drills without
through tool coolant can drill up to five times diameter deep in carbon steels and aluminum
before needing to peck drill. The problem with peck drilling
is that most tool wear occurs when the drill is
entering the material. Once the drill is in the cut,
wear rates become very low. Peck drilling significantly
increases tool wear because you're restarting the
cut multiple times per hole. Not to mention all the extra
time spent pecking each hole where the TSC drill would
do it in just one pass. So for tools more than five times depth and particularly when drilling tough or work hardy materials,
TSC and through tool drills really become a necessity. If you need to drill very deep holes, let's say eight times diameter or greater, you'll usually need a pilot
hole to start the drill. Typically this is done
by using a stub drill to cut the hole about one and
a half times diameter deep. Then start the long drill with a spin let 300-500 RPM, and slowly
feed it into the pilot hole. Once the drill main diameter
is in the pilot hole you can crank up the RPM to full speed and finish drilling to full depth. When drilling holes that
break through the work piece, pay special attention to the material and cutting conditions. Drill manufacturers recommend
slowing the feed rate before the drill point breaks through the material to prevent chipping and reduce heat in the cut. We wanna reduce the heat because as the drill gets to the very bottom, before it breaks through, the material is very thin and there is no place for the heat to go. So that last bit of
material can work harden, literally heat treating the material. Breaking through this heat treated layer can shorten the life of the drill. A 50% reduction in feed rate for the final two millimeters or 0.01" before the drill point reaches the bottom usually eliminates this issue. So when does a drill need to be sharpened? Generally speaking, as long as your holes are in tolerance, if wear and chipping are less than half a millimeter or 0.02" it's okay to continue using the drill. After that it's typically time to resharpen or regrind. Pay close attention for
chipping on the drill margins. If the wear is even, it's okay to regrind. But if it looks like this,
the drill is no longer useful. Now often times you'll be buying tools and deciding what you should spend at a specific job. Is it a short one single lot? Or is it a large recurring
job with thousands of parts? Carbide might not be the best investment if you've got a short run and you can't spend extra time dialing
in your cutting parameters. High-speed steel or cobalt
might make sense in this case. Keep in mind that you can always start with less expensive drills
to get the job launched. Then if you end up
making lots of those same parts down the road,
you can work with your tooling supplier to find
the best tool for the job whether it's carbide or
a high end cobalt drill. So let's do a lightning fast recap. Carbide is much more
expensive than the others. It's also less forgiving
if used incorrectly. High-speed steel and cobalt
are easy to resharpen but don't offer anywhere near
the tool life of carbide. Typically, carbide can also
run significantly faster. When it comes to coatings,
if your machining difficult materials or need max tool life for long part runs, then
select the high end coatings. And for geometry, we're just
touching on some of the aspects but consider the material and
your cycle time requirements when deciding which way to go
with each of these elements. If you have questions or comments about how drills have worked in
your specific circumstances, let us know in the comments section. And don't miss the opportunity to tap into the expertise of your local tooling rep. They've got the insider knowledge
on using their tools best and will get you on the right
track for your application. Thanks for watching this
first episode of Haas U. And we'll see you next time.
Pretty interesting ngl lmao before I knew it i watched the entire 15 mins
Awesome vid. just cleaned up my drill press today and was checking through the bits, seems to be all basic stuff. These guys are pros.
Basics of Drill Selection - AvE University
Did anyone else notice the flux capacitors sign?
What they don’t mention in the negatives of HSS is that when you inevitably break the tool, HSS likes to go looking for your eyes. Carbide just sort of snaps and falls harmlessly. Most machinists I know with home shops pretty much only use carbide at home.